Modeling tool

Extrude

Give depth to one or more closed sketch profiles or planar model faces, creating or modifying solid volume.

Purpose#

Give depth to one or more closed sketch profiles or planar model faces, creating or modifying solid volume.

Where to find it#

Select closed profiles or planar faces in Model, then choose Create > Extrude.

Selection#

• Select one or more closed, non-self-intersecting sketch profiles or supported planar faces.
• For Join, Cut, or Intersect, also choose the target body when MakerSolid cannot resolve it unambiguously.

Steps#

1. Select closed profiles or a planar source face and open Extrude. Distance remains the default end condition and starts with a round value in the project unit.
2. Open Details for end conditions, offsets, custom directions, or independent sides. The command bar keeps the Distance input for distance-based extrusions.
3. In Details, Distance, Per-Side Distance, End Scale, Twist, Start Offset, Clearance, and Shape Reference Length keep their labels above precision inputs. Tap a value to enter a number or expression, or drag its scrubber horizontally to adjust; vertical position changes precision. Lengths use the current project unit. Expression-backed values keep their link and must be edited through the keypad.
4. Choose the start, direction, sides, and end. Use the dedicated picker to select a termination face or body without replacing the source profile.
5. Choose Operation and its Target independently of the termination reference. Distance, End Scale, and Twist update the affected-volume preview immediately. For referenced starts, ends, or directions, wait for the exact preview to succeed. Tap Apply to build and validate the final result.

Options#

Distance

#

Sets signed extrusion depth along the profile normal; the sign reverses direction. If you switch to a referenced end and then return without changing other extent settings, MakerSolid restores the original Distance and its Join/Cut affected-volume preview.

ƒ Accepts variables and expressions

Symmetric

#

Uses the entered distance on each side of the profile plane. The structured extent editor labels this Per-Side Distance.

Merge profiles

#

Unions compatible selected profiles before extrusion so overlapping regions are treated as one source.

End Scale

#

Scales the end section relative to the start to create taper-like geometry; 1 keeps the same size.

ƒ Accepts variables and expressions

Twist

#

Rotates the end section by the entered angle across the extrusion distance.

ƒ Accepts variables and expressions

Operation

#

New Body creates a separate solid; Join adds to Target; Cut subtracts from Target; Intersect keeps common volume.

New BodyJoinCutIntersect

Target

#

Chooses the body modified by Join, Cut, or Intersect.

Available when: Shown when Operation is not New Body.

Details

#

Details directly shows grouped Start, Direction, Sides, End, and Shape controls, including the End condition selector. The command bar retains the Distance input for distance-based extrusions. Existing saved extrusions retain their original geometry until edited. Numeric inputs in Details and the Extrude History editor provide a keypad and scrubber below their labels.

Start

#

Profile Plane starts at the source. Start Offset translates the profile along the chosen extrusion direction. A selected face or plane trims the sweep without wrapping or deforming the source profile.

Profile PlaneOffsetSelected Face/Plane

ƒ Accepts variables and expressions

Direction

#

Use the profile normal, a world or construction axis, a straight model edge, or explicit X/Y/Z components. Zero vectors and directions parallel to the profile plane are rejected.

Profile NormalReverse DirectionExplicit VectorPick Axis or Straight Edge

Sides

#

Two Sides exposes independent end conditions, scale, twist, and reference length. Symmetric uses a distance on each side.

One SideTwo SidesSymmetric

End Condition

#

Face termination uses the actual trimmed face, including curved loft faces; it does not extend the surface. Construction and world planes are infinite. Body termination can span several boundary faces. End Body and candidate-body choices use the same labels shown in the Bodies browser, including renamed bodies. Next uses the first encountered boundary, or the first exit when the source starts inside a candidate body. Through All spans the candidate bodies and is available only for Cut and Intersect.

DistanceUp to Face/PlaneUp to BodyUp to NextThrough All

Candidate Bodies

#

The body toggles for Next and Through All save the selected candidate set. Later visibility changes do not change the saved termination.

Available when: Shown for Up to Next and Through All.

Clearance

#

Positive end clearance stops short; negative clearance extends past the target. Along Extrusion translates the boundary; Normal to Surface offsets its surface. Positive start clearance moves the referenced start into the interval. Invalid or singular offset geometry is rejected.

Along ExtrusionNormal to Surface

Available when: Shown for referenced starts and face/body/Next ends.

ƒ Accepts variables and expressions

Shape Reference Length

#

For a referenced end, scale and twist reach the specified values at this positive axial length. Those laws continue beyond that station until the target trims the sweep. The whole interval must keep positive scale. Numeric start offset moves the deformation origin; referenced starts trim without resetting it. Distance mode keeps its end-section scale and twist interpretation.

Available when: Shown for non-distance ends.

ƒ Accepts variables and expressions

Cancel Selection

#

Exits the current start/end/direction picker while retaining the extrusion inputs and source selection. Pick Start Face, Pick End Face, and Pick End Body replace only their named reference.

Result#

Apply adds an associative Extrude feature using the selected profile or face references.

Editing#

Open Extrude in History to edit the saved definition, operation, or boolean target. The Result card labels Operation and Target Body; Target Body appears for Join, Cut, and Intersect. Numeric parameters, including Distance, End Scale, Twist, and Clearance, use labels above their inputs so the names stay readable in the narrow pane. Tap a numeric value to open the keypad, or drag its scrubber to adjust it using the project precision. The keypad retains invalid expressions for correction and enables Apply value only for valid input; the saved feature is unchanged until Update Feature. Reversed definitions show Reverse Direction with a positive Distance. Lengths display and accept the current project unit inside each control, so 1 in reopens as 1 in. Reference picking shows upstream geometry; a construction plane or axis derived from the edited feature or later history must be replaced with an upstream reference. Distance, End Scale, and Twist update the affected-volume preview immediately while you edit. Boolean edits keep the committed body visible as dimmed context, and the affected volume follows later Move, Rotate, and Scale operations. Histories with other dependent operations use an exact preview. Distances preserve the entered length; temporary cutting margins do not change the saved value. Older plain face cuts with a verified padded profile recover their original Distance when opened in History and save the correction with Update Feature. Update Feature builds and validates the final result, including downstream features. Referenced starts, ends, and directions require a successful current exact preview before Update Feature is enabled. Invalid inputs remain editable; a failed update does not change the saved project. Legacy symmetric scaled/twisted extrusions convert to an equivalent offset sweep to preserve their deformation origin.

Troubleshooting#